What Am I doing wrong? Help !

Hello all,

I just got my new handibot the other day ! (Thank you guys !! ) I'm Very Excited, And I have been trying to learn the V-Carve software, I've been reading what I can, as well as watching videos.. I got it do a test program on doing some texts, and it worked fine.. even did a small profile, just to see how it would work out.. well it was taking too deep of a pass, I'm cutting 1/8 thick copper.. So I stopped the program, and started over in V-carve to change the depth passes...Done.. I save the new file , And now when I send it to the Handibot to run, it asks me to change the tool, i hit the green button again, and it starts the spindle up and rapids to its starting location, and does what looks like a drill or spot drill cycle, goes about .010 deep, and rapids to another location, does it, rapids again, and does it again..then the program stops..Now what I am seeing on the V-carve program ( the drawing and toolpaths) is not doing any of that.. This is happening now with everything i do, I tried starting a new file, and do some text. Does the same thing, but the spot cycle (that's what I'm calling it i guess) happens again, but its within the area that the text is suppose to be, and only one quick spot, then the program ends... So I try the " hole cutter App " After I enter the info it requires, I run it, same thing happens.. it rapids to my start location, z rapids down to its start point, feeds down and does a quick spot, and rapids up and program ends... Now this is a new machine for me, and I don't think I screwed anything up any where, but if theres something I may not be doing right, I'm looking for advice, or has this happened to anyone else that figured out what was going on?

Sorry for the noobie question.. lol

Thanks all

Rob

Rob,
when I first started reading I thought maybe you had set something wrong in vcarve but no, if it is doing it using the code from the hole app then it is a machine problem. First thing with any digital machine problem is to shut it down, way down, all the way off, and unplugged. then bring it up and see if the problem persists. if it does, the FabMo card probably needs to be reloaded. If it is not too far gone you can flash the ROM yourself. There are instructions on the main site. If it is too far gone they might have to swap cards with you but that is easy as well.

When things get like this, I always suggest calling them during normal working hours. They are SUPER helpful.

One last thought. While the handibot will cut brass and aluminum just fine in very light cuts I'd suggest getting to know her with several projects in wood before going there.

Ok Mark, What Ive done also last nite was updated the macro, and that didnt help. Its still doing the same thing.. So I also unplugged everything and ran some errands this morning ( took the day off from work ) When I can back home, I plugged everything back in and fired her up.. And shes still doing the same thing. When I'm on the Fabmo app, I can edit the program I want to send, so While I'm looking at that program, Its showing a lot of code and movements.. But what the machines actually doing is different.. like I said, It starts up, goes to a position, does a quick z move down then back up and rapids to its zero location and stops..

I also cut a couple of these profiles on some wood when I first got the machine last week, When I started to try the copper, it ran fine, just needed more depth passes, so it wasn't taking so much in one pass.. I make lots of Parts on my HAAS Machines at work, but I can hog out much more material at a time, so knowing that the handibot is much much smaller, I know to be easy on it when machining some soft metals...

So i'm going to try and reload the Fabmo card as you said. I'll look those instructions up on their main site, and give it a shot.. if not, I'll be calling them up and see what the next step is... As much as its cool to have this wireless, I wish there was a usb port on the machine itself in case one didn't want to use the wireless function. I know its a great feature.. and I do like it, but if the wireless part is not working, then its good to have another way..

Thanks for your help, and I'll post up here what happens next..

Rob

Rob,

I've been messing around in the shop here today trying to recreate your problem to see what might be causing it. I'm using the same software version and macros as you and haven't been able to trigger the error on my tool.
I also performed a reflash of the card; following the directions on our website--I realized that there is a step missing from those instructions--once the reflash is complete and you plug your card back into your tool and power the tool on...you'll need to let it sit for about 10 minutes while it unpacks a few last updates and installs them. After that, power cycle to tool to activate the engine.
I'll keep digging here to try to figure out if there is a setting that might be causing your error.

Brian

Brian,

Thank you for responding to this issue. I really appreciate it... Ok, I've re-flashed the card per the instructions your site gives, ( I love the instruction layout, easy and right to the point ! as with all of your doc's) So I'm just waiting on the 10 minute time period that you suggested, and I'll turn off the machine, and start her back up again.. I hope this resolves it.. :/ I will post here what happens..

Rob

Ok, I've fired her up and ran a simple program profile... and she keeps doing the same thing... Kinda frustrating...

Should I give you guys a call? I see your only open until 5pm and its 4:05 right now. If I call tomorrow it will be from my work, and I wont be able to give much info on the machine from there, and wont be home till 4pm.. Maybe it needs a new Fabmo card?



Rob

Rob,

I'm studying the /log file that you sent--(for those who don't know, you can access the log of all commands processed by your tool by adding /log after the IP address in the browser e.g. 192.168.42.1/log). There is definitely something weird happening at the software level. Each line in the files that we ran is showing an error of "FEEDRATE NOT SPECIFIED"--which makes sense--because you describe the error as the tool jogging into position, skipping the cut, and jogging back home. "Jog" moves don't require a feedrate, but "Move" commands do--so the tool is able to do the jogs, but skips all the moves.

I've posted this to our internal chat here for some more information--I'll follow up here as soon as I know something.

The typical header of a file will look something like this:

IF %(25)=1 THEN GOTO UNIT_ERROR 'check to see software is set to standard
SA 'Set program to absolute coordinate mode
CN, 90
'New Path
'Toolpath Name = Pocket 1
'Tool Name = End Mill (0.0625 inches)

&PWSafeZ = 0.200
&PWZorigin = Material Surface
&PWMaterial = 0.500
'&ToolName = "End Mill (0.0625 inches)"
&Tool =72 'Tool number to change to
C9 'Change tool
TR,14000 'Set spindle RPM
C6 'Spindle on
PAUSE 2
'
MS,3.0,1.0

Really the only commands needed to initialize a file are "C6" which starts the spindle--and PAUSE 2 which gives the spindle time to spin up before running. "MS,...." sets the feedrates for the X,Y and Z axes. The rest can be commented out by placing an apostrophe at the beginning of those lines. It would be interesting to see what happens with just the C6, PAUSE, and MS commands in a header.

So, I think I've finally gotten to the bottom of this one! Had everyone here scratching their heads for a while.
I got ahold of this code that was being submitted to the tool:

'----------------------------------------------------------------
'SHOPBOT ROUTER FILE IN INCHES
'GENERATED BY PARTWorks
'Minimum extent in X = -2.500 Minimum extent in Y = -2.500 Minimum extent in Z = -0.125
'Maximum extent in X = 2.500 Maximum extent in Y = 2.500 Maximum extent in Z = 0.000
'Length of material in X = 5.000
'Length of material in Y = 5.000
'Depth of material in Z = 0.125
'Home Position Information = Center, Material Surface
'Home X = 0.000000 Home Y = 0.000000 Home Z = 0.800000
'Rapid clearance gap or Safe Z = 0.200
'UNITS:Inches
'
IF %(25)=1 THEN GOTO UNIT_ERROR 'check to see software is set to standard
SA 'Set program to absolute coordinate mode
CN, 90
'New Path
'Toolpath Name = TESTPRT
'Tool Name = End Mill (0.063 inches)

&PWSafeZ = 0.200
&PWZorigin = Material Surface
&PWMaterial = 0.125
'&ToolName = "End Mill (0.063 inches)"
&Tool =1 'Tool number to change to
C9 'Change tool
TR,14000 'Set spindle RPM
C6 'Spindle on
PAUSE 2
'
MS,0.0,0.0
JZ,0.800000
J3,0.000000,-0.281502,0.200000
J3,0.000000,-0.281502,0.000000
M3,0.000000,-0.281502,-0.032500
M3,-0.032801,-0.281170,-0.032500

....
Now if any of you are familiar with ShopBot code--try to spot something out of the ordinary before continuing...


give up?
Check out the MS command right after the spindle is turned on by the C6 command. MS is short for move speed and it passes the feedrate data from your tool profile in vcarve to the FabMo control software. MS, 0.0, 0.0 tells the tool that the feedrate should be 0 inches per second in the X and Y axes, and 0 inches per second in the Z axis. In the old ShopBot software, this would generate a warning that wouldn't allow you to continue with the cut until the move speed was at least 0.05 ips in every axis. Currently there is no such warning in FabMo. Instead, it will commence the cut, it will even move a little bit because the first few moves in the file are Jogs (high speed moves) which have their own speed settings with defaults in FabMo. As soon as it gets to the first move command (M3, ..., ..., ...) it can't find a speed value so it skips every move all the way to the end of the file where it jogs home and turns off the spindle.

The fix here would be to edit the tool profile in vcarve with a non-zero value for feedrate and then recalculate the toolpath and save a new copy of the file. In a pinch you can also just edit the MS command in the code.

This is why the problem seemed intermittent. Running files from certain apps would put a speed value into the system and things would run correctly. Other apps that didn't specify speed would just use the values left over from previous runs. However, when one of the vcarve files would run, it would wipe out the speed values...and any app that didn't specify its own speed values would also stop working.

Anyway--this was a great puzzle and we all learned something here in trying to solve it! We're trying to decide how best to implement warnings about speed values in FabMo now. Can anyone think of a reason that you'd want a zero speed for a toolpath??

Brian

Thats definitely It ! And the program works after I edit the code... But I have filled out the field for feedrate in v-carve, and after I save it and post the program, It still comes out with those values missing.. So the only way it works is I have to edit it.. It should come out when its posted from V-carve... Whats weird is.. the message above, you copied what I sent you, and there is a Value after MS its MS,3.0,1.0 But it wasn't working then either, so either way... I'm glad you guys narrowed it down to that, and it wasn't a hardware issue. And it makes complete sense as to why it was doing what it was doing..


If I haven't mentioned it, I'd like to say again, Brian, thank you for helping me out so far, I really do appreciate it.. right here, you have a customer for life.. I looked at many other CNC desktop machines before this purchase, and it was for much cheaper ones, and By far, I definitely made the right choice..

Also Mark, if your reading this.. I appreciate your help as well, As I look through the forum here, you have helped out so many people..

The only other problem i see from here on out, is trying to keep this great looking machine clean.. LOL

Rob